Complex modelling approach

[SirEngineer]

Hello - was wondering if anyone would give me a few pointers. Wanted to learn Fusion 360 a bit, looked around and decided to draw one of my screwdrivers. Struggled a bit on how to actually model it and below is my attempt along with a picture of the actual screwdriver. If you look at the screwdriver, on each face is an inner profile. I extruded that and again at 90 degrees to itself. I then extruded the outer profile 'intersect' with the two inner profiles a both plan and 90 degrees if that makes sense. I then used 'loft' to fill in the hexagonal gaps between the inner and outer profiles - the faces at 45, 135, 225 and 315 degrees if looking from the end.  

Then extruded the hexagonal end cap where the blade goes and as it appears I missed the non-blade end cap, I revolved that but didn't do a great job. I was then hoping to 'fillet' the sharp edges but Fusion 360 won't allow me to, not sure why. Anyway, how would any advances users model this object? I'm sure there must be a better way but my limited modelling ability isn't aware if it

[SirEngineer]

Model attached

[SirEngineer]

Model attached....

[SirEngineer]

Hello - I'm still stuck on modelling the dimple/thumb detent area in each of the screwriver's faces. I've tried so many things - revolve surfaces on difference axis, extrude profiles etc, but nothing doing. Any tips?

[SirEngineer]

Hello - I'm still stuck on modelling the dimple/thumb detent area in each of the screwriver's faces. I've tried so many things - revolve surfaces on difference axis, extrude profiles etc, but nothing doing. Any tips?

[kb9ydn]

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@SirEngineer wrote:

Hello - I'm still stuck on modelling the dimple/thumb detent area in each of the screwriver's faces. I've tried so many things - revolve surfaces on difference axis, extrude profiles etc, but nothing doing. Any tips?

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Could you post a clearer picture of the dimpled area?  It's hard to see in the first picture.

C|

[ritste20]

I wouldn't call this a beginner approach by any means but after you explore the process that @TheCADWhisperer is shepherding you through, something else to consider would be the form tools. A lot of complex geometry can be accomplished without being constrained to planar operations like extrude, cut, sweep, etc...

A word of caution, if you are not careful with form tools it is easy to create horrible curvatures that are not manufacturable. But once you are more comfortable with solid modeling operations you can find plenty of youtube videos that explain the different manipulations possible in the free-form environment.

Regards,

[PhilProcarioJr]

@SirEngineer 

This is a pretty simple way to approach this, see if it is what you are after.

[SirEngineer]

Thank you so much, thats brilliant. I have downloaded your model but can't quite see how you did what you did even though I've played back the commands/events etc? I will investigate more - thank you

[SirEngineer]

Wow - that's brilliant - and I can see playing back the events how you created two offset planes, drew the loft path and then split the faces, deleted the faces too. I am pretty sure with a bit of mucking around I can duplicate that too, so it's brilliant - thank you. I get the feeling you reproduced the model in a few minutes though.... wheras I've spent hours and hours. Still, great way to learn Fusion 360 by doing things/challenges so it's been fun

[PhilProcarioJr]

@SirEngineer 

If you need any further explanation just let me know. I wanted to keep the modeling clean and as simple as possible.

I think I spent maybe 2-3 min making the model. I didn't focus on making the scale correct as you only asked how it could be modeled.

If this answered your question can you mark it as an accepted solution? I would appreciate it.

Best regards,

Phil

[ritste20]

That's both the beauty and beast of form tools. While editing the form you can use the undo command so there is a history recorded but not in an editable fashion like you would see on the timeline when using the solid modeling operations. Once you close the file, the undo history is gone so the only way to change something back is again to manually manipulate the model. Form tools provide an infinite level of customization down to individual vertices if required which is also why it is easy to mess things up.

Again, not a beginner approach but the options are there as you get more comfortable with operating Fusion and want to try more complex models. Every tool is good to have in the toolbox, once you know how it works.

Regards,

[SirEngineer]

I'm struggling with the loft command. I've done what I can see you have done (not familiar with the splines?) but have created both outside and midplane curves. Now to loft between them, I've been looking at tutorials but they all seem to loft closed shapes like circles etc. I can't seem to properly select the curves/lines I've used for the shapes, if I window everything then it treats each individual line/curve as a different profile, wheras I see on yours each one is somehow connected. Also even though all those sketches are visible, when in the loft command they don't seem to be selectable?

[PhilProcarioJr]

@SirEngineer 

If you are under the Solid tab then you can not select the curves, you have to be under the Surface tab.

[ritste20]

Since you are trying to create a lofted surface from lines and spines (no closed profiles), make sure you are using the loft operation on the surface tab, not the solid tab.

If that isn't the problem you're experiencing a screencast recording would help to diagnose what is going on.

Regards,

[SirEngineer]

Progressing! Great, that makes sense. However my curves are a combination of splines and straight lines/arcs, when selecting them with loft it treats each as separate paths. I see you have used all splines and the loft command selects all connected lofts as one. Guess I need to re-do the sketches with all splines?

Don't know how to screenshot record!

[PhilProcarioJr]

@SirEngineer 

You can use arcs and lines as one profile as long as you constrain them as G1 tangency (if they are not set to tangent Fusion will do what your talking about), but splines are easier to use and control for something like this.

[SirEngineer]

ok, will re-do, I see more how you did them. Then the Split Face command, selecting the faces and using the loft as the Splitting Tool, then delete the area inside the loft? Thank you a million for your help too

[PhilProcarioJr]

@SirEngineer 

Make sure after you split the face and duplicate the surfaces that you stitch the surfaces back together at the end to create a solid again so you can fillet everything.

[SirEngineer]

Ahh! so that was the reason for the stitch command in your sketch. I've got the loft working, seems F360 lets me add more of my lines once the loft has been done if that makes sense. Is there an easy way to create the second (mirror) plane/sketch once the first outside one has been done. I have CTRL C the sketch then select the second plane and CTRL V but it pasts back on the first plane. Ideally it would be a copy of the first plane anyway and parametric?

[PhilProcarioJr]

@SirEngineer 

What you want to do is create a sketch on the second offset plane and hit the P key to enable projection, then select the spline, arc, lines from the other sketch and it will duplicate them and your done. This method will also keep it parametric so if you modify the first spline the second sketch will automatically update.